CNC milling DFM checker, eight feasibility checks before you commit to a cut

A milling tool is a round cutter, so the corner it leaves between two pocket or slot walls always carries the same radius as the tool itself: a 10 millimetre diameter tool has a 5 millimetre radius, and no toolpath trick makes it sharper than its own geometry. That makes the minimum internal radius on a drawing a physical limit, not a preference. In practice the safe margin is a little wider than the bare minimum: cutting at exactly the tool radius means the tool engages with almost its full side surface in the corner, which raises heat, wears the edge faster and invites vibration, so published design guides from Fictiv, Xometry and Protolabs recommend a radius at least 20 percent above the tool radius.

A milling tool is only held at one end, in the spindle, so the deeper it cuts relative to its own diameter, the more it deflects under the cutting force, an effect you cannot see but that shows up as an undersized wall, a wavy surface or outright chatter. Up to 3 times the tool diameter a standard solid carbide end mill cuts at full rigidity. Between 3 and 5 times the deflection grows quickly, so the checker calls for slower feed and a lighter stepover at each pass. Past 5 times a standard tool is no longer a sensible choice, and the recommendation becomes a specialised extended-neck tool running much slower.

A thin wall is the mirror image of a deep pocket: instead of the tool deflecting, the part itself flexes sideways under the cutting force, and past a certain point the flex turns into vibration that leaves visible marks or breaks the wall during fixturing. The minimum published thickness for milling is around 0.5 millimetres for aluminium and steel and around 1.0 millimetre for engineering plastic, because a lower modulus of elasticity needs more material for the same stiffness. That is a different limit from the wall's height to thickness ratio: a wall can sit comfortably above the minimum thickness and still be tall and flexible enough to chatter, which is why the checker treats the two as separate rules rather than one.

The first limit is how deep the thread has to engage to carry its rated load, and that depends on the part material rather than the screw: engineering tables call for roughly 1.5 times the nominal diameter in steel, 2 times in aluminium and 2.5 times in plastic, because a softer material shears more easily and needs a longer engagement to reach the same strength as a steel thread in a steel part. The second limit is unrelated to strength: it is how deep you can practically cut a thread with a tap before the risk of snapping it off in a closed hole becomes real, which depends mostly on chip evacuation, not material. Standard tapping stays comfortable to about 3 times the diameter, needs a spiral flute tap and a slower cycle up to about 4 times, and past that the checker points towards thread milling or a through hole instead.

A milling tool cuts in a straight line from its current approach direction, so anything hidden behind that direction is out of reach regardless of size. The checker separates three degrees of the problem: a profile the tool cannot cut with a plain cylindrical shape, such as a T slot or dovetail, which just needs the right form tool in the same setup; a feature on a face the current approach cannot see at all, which needs the part refixtured on a new setup with its own position tolerance against the rest of the part; and a fully enclosed cavity that is wider inside than at its own opening, which no number of setups can fix, because the limit is the shape itself, not the direction, and the only way out is a different process or a redesign.

Take an aluminium part with a 28 millimetre deep pocket cut with an 8 millimetre tool. The depth to diameter ratio is 28 divided by 8, or 3.5, above the 3 to 1 rigidity threshold and below the 5 to 1 practical limit, so that check reads warn with slower feed along the pocket walls. The same pocket carries an internal corner with a 5 millimetre radius: the tool radius is 4 millimetres, the recommended radius is 4 times 1.2, or 4.8 millimetres, and 5 is above that, so the corner radius check reads ok. A wall between this pocket and a neighbouring hole is 0.7 millimetres thick: above the 0.5 millimetre aluminium minimum but below the 0.8 millimetre recommended figure, so that check reads warn as well, because the cutting force can flex it on the final pass. Three checks on one part, three different verdicts, which is exactly why the checker reports each one on its own instead of a single combined score.

No, and it says so on the page itself. There is currently no verified rules engine inside EduFacturing for CNC milling the way there is for laser cutting, so every number here is a catalogue value from a published source stated under its own result: design guides from Fictiv, Xometry and Protolabs, application notes from Sandvik Coromant and Harvey Performance Co, and reference tables from Machinery's Handbook and the Fastenal Technical Reference Guide. That makes this a starting point from shop floor practice, useful for a first pass on a drawing, not a substitute for a conversation with the shop that will actually cut the part, especially with a tight tolerance, an unusual material, or several borderline rules combining on the same feature. The added cost percentages are the tool's own engineering estimate, not a supplier price list, and a warn or invalid on one rule out of eight still means the drawing needs a second look before it goes out for quote.